Thermoforming Tolerances: What a Formed Part Can Actually Hold

Why a formed part cannot hold a moulded tolerance

The first conversation about a thermoformed part is usually about tolerance, and it usually starts with a drawing carried over from an injection moulded version of the same product. The numbers on it are ±0.2 mm and the former says ±1.5 mm, and both parties think the other is being unreasonable.

Neither is. Injection moulding holds tight tolerances because the cavity is steel and the part is a copy of it, shrunk by a known and repeatable amount. Thermoforming holds looser tolerances because the part is a copy of a mould made from a sheet that was itself variable, stretched by an amount that depends on where on the sheet you look, and then cut off the sheet by a trimming operation with its own error.

The tolerance on a formed part is the sum of five independent errors, and only one of them is under the former's control at the machine.

Table 1 — The five error sources on a formed part. The first one is usually the largest and is almost never discussed.

Sheet thickness variation is the one that surprises people. A 3 mm sheet supplied to ±5% is 2.85 to 3.15 mm, and that 10% range propagates directly into every formed feature whose height depends on how much material was there. It also changes the stretch ratio, so a thin patch of sheet forms a slightly different shape from a thick patch of the same sheet.

The tolerance stack, worked through

Take a 400 mm long formed cover in ABS, 3 mm sheet, trimmed on a CNC router. The drawing says ±0.5 mm on the overall length. Here is why that cannot be met and what can.

Table 2 — Tolerance stack for a 400 mm ABS cover. The sum of independent errors is smaller than the arithmetic total but far larger than ±0.5 mm.

Note the shrinkage line. It is by far the largest single number, and it is also the one that can be removed: scaling the tool by 1/(1−S) compensates the mean shrink exactly, and what remains is only the batch-to-batch scatter, which is the ±0.3 mm. That is why tool scaling matters and why arguing about trim accuracy first is arguing about the wrong thing.

What a former can actually hold

Table 3 — Practical tolerances by dimension type and size. Wall thickness is a percentage, not an absolute, and it is the tolerance that catches people out.

Two rows deserve comment. Wall thickness is not a dimension the former controls in the usual sense — it is a consequence of the draw ratio, and a deep draw will thin the wall at the bottom corner by 40% no matter what the drawing says. It has to be tolerated as a percentage with a minimum, and the design has to accept it.

The other is "feature on side wall to feature on base". This is a cross-plane dimension, and it accumulates the spring-back of two faces plus the trim of two edges. It is where drawings most often specify an impossible number, usually because the part was previously machined from solid.

Shrinkage, and the scaling factor

Every material has a forming shrinkage, and the tool has to be scaled by 1/(1−S) to compensate. The number is not the same as the moulding shrinkage quoted on the datasheet, because a formed part is constrained by the mould during cooling in a different way.

Table 4 — Forming shrinkage and the resulting tool scale factor. Polyolefins are the reason a first article matters.

Polypropylene is the material that punishes optimism. Its shrinkage ranges over nearly a full percentage point depending on grade, nucleating agent and cooling rate, and 1.5% on a 500 mm part is 7.5 mm. No tool scale can be right for the whole range, so a PP part either accepts a wide tolerance or the tool is cut after a first-article trial on the actual resin batch.

That is standard practice and worth stating plainly: for a new PP or HDPE part, the tool is cut slightly undersize, a trial part is measured, and the tool is adjusted or a second tool is cut. Budgeting for one tool iteration on polyolefin is cheaper than accepting a part that does not fit.

Trimming: the biggest single lever

Of the five error sources, trimming is the one the former can change most easily and the one that most affects the tolerance a customer actually experiences, because the trimmed outline is the dimension that has to fit into an assembly.

Table 5 — Trimming methods. Moving from hand trim to a CNC fixture typically buys 1 mm of tolerance for a few percent of part cost.

The most common mistake is specifying a tolerance that requires a CNC fixture and then not paying for the fixture. A part trimmed on a 5-axis router without a dedicated fixture moves by a millimetre or more between cycles, because the formed part does not sit in the same place twice. A fixture that locates on two formed features rather than on the trimmed edge is what turns ±0.8 mm into ±0.3 mm.

For thin-gauge packaging, the economics invert. A steel trim die costs real money but runs at a cycle time measured in seconds, and at a million parts the per-part cost is negligible. For heavy-gauge industrial parts at a few hundred a year, a CNC fixture is the only sensible answer.

Datum strategy: how to make the number measurable

Most tolerance disputes are not about capability. They are about which surface the measurement was taken from, and a formed part has no natural datum.

A machined part has a flat face that can be put on a surface plate. A formed part has a draft angle on every wall, a radius at every corner, and a trimmed edge that is not perpendicular to anything. The first thing to agree is the datum scheme, and it should be on the drawing before the tool is cut.

The practical scheme for most formed parts is: primary datum is three points on the largest flat face; secondary is two points on the longest straight trimmed edge; tertiary is one point on a second trimmed edge. That is a standard 3-2-1 location and it is measurable on a CMM or with a height gauge and a fixture.

What does not work is calling out the inside of a formed pocket as a datum when the pocket has a draft angle, or calling out a trimmed edge as a datum when the trimming method is hand trim. Both produce a drawing that cannot be inspected, and an inspector who invents a scheme, and a batch that is rejected for the wrong reason.

Table 6 — Drawing practices that cause disputes, and what to write instead. The temperature row is the one that produces arguments in July.

Thermal expansion deserves the emphasis. A metre of PMMA moves 0.7 mm over 10 °C, which is larger than most of the tolerances being argued about. A part formed in a warm shop, measured in an air-conditioned inspection room two hours later, and compared against a drawing with no reference temperature is a measurement of the weather, not of the part.